We sometimes need to define a thruhole via as a stack up of blind microvias and buried vias. This is becasue on th eTop and Bottom layers I need a smaller pad, that cannot be acieved with thruhole via, but only with blind micorvias. Is it possible in PCB Editor to define such a via, or at least to place a via over another in this way?
I'm an experienced self-taught on Orcad Layout 10.5, and I'm in the process to change to PCB Designer 16.6, and I find it very difficult to mentally 'translate' old Layout commands and names to PCB editor, they are so different!
Thanks in advance,
If I understand your goal then it is easy to achieve. When you create a via padstack using the Pad Designer you can define the pad size for the top layer, the bottom layer, and the internal layers separately.
In reply to BuddSw:
Not so simple, I want it to be constructed with different drill sizes also, but the PAD Designer only allows one drill for the whole via.
In reply to Leticia:
Sorry. I missed that you needed different drill sizes also.
Have you tried Setup->B/B Via Definitions using different seed vias.
In reply to aCraig:
HI Craig, thanks, but what do you mean with different seed vias? I want to put all of them in the same place.
You mentioned that you need padstacks with different drill sizes stack on top of each other. So you will need to create a seed padstack for each drill size, then use those padstack to seed the bbvia.
I'm sorry, I don't understand what a seed padstack for each drill size means. Could you explain it for me please? Thanks in advance
To create a bbvia you need an input padstack inorder to build bbvia from, that's the seed padstack. If you look at the dialog for creating bbvia it will as you for an "input padstack".
Thanks Craig, but my doubt is how do I place one via over another, or better, how do I define a via as the joint of two or more previously defined vias.
I try to place a blind via from top to In1, over a buried via, fro In1 to In4, but the DRC does not allow me to do this. Even if I could manage to do this, this is not the ideal solution, I would like to be able to create a via and define the drill size between each pair of layers, I don't see anything like this in the software, but I'm very new at it, so it may exist and it's just that I can't find it.
Thanks again for your answers,
You should download the Allegro HDI Best Practices paper, this can be found at http://support.cadence.com
For stacked vias, start in the Physical domain of Constraint Manager.
Set Pad-Pad Connect for the common layer of the stacked series of vias to
L3, L2 is the common layer.
Once vias are stacked, slide will treat them as a single entity. Use the RMB to split the stack if necessary. The Via label will display the stack in this example as 1-3.
There is a Best Practices document for High Density Interconnect Design which covers the use of Microvias, here is the link to it on the support site.
In order to use Microvias you need the Allegro PCB Designer license with the Miniaturization option to give you the enhanced functionality.
Hope this helps,